[bigphil]

Originally Posted by Neb

Hi,
I am installing the FSI foam extend 4.1 toolkit on Ubuntu 18.04. I have already fixed many bugs and used the gcc-5 compiler. Now I have last errors.
I would be very grateful for your help!

Ah, you are using FSI from the extend-bazaar, I thought you were using solids4foam.

I suggest you try solids4foam (https://bitbucket.org/philip_cardiff...se/src/master/) instead as the extend-bazaar code was integrated into it and the extend-bazaar code is no longer actively supported.

[Neb]

Originally Posted by bigphil

Ah, you are using FSI from the extend-bazaar, I thought you were using solids4foam.

I suggest you try solids4foam (https://bitbucket.org/philip_cardiff...se/src/master/) instead as the extend-bazaar code was integrated into it and the extend-bazaar code is no longer actively supported.

Thanks for your reply and for your suggestion. I switched to solids4foam and did some tutorials, it works great!

[Neb]

Hi,

I have to solve some problems for an FSI simulation with solids4foam.
1) how can I create a new boundary condition for the fluid region? Is there such a thing as OpenFoam's codedFixedValue?
2) for the postProcess I need the WallShearStress, Q, yPlus, turbulence intensity. How can I get them?
3) is there a functions to insert in controlDict to calculate the average flow rate and pressure at the outlets?

Thank you

[danielparmar]

I recently started working on a project related to FSI of flexible wings. I am using turekHron fsi case from solids4foam. Since for flexible wing, atmospheric conditions are needed. Thus I have changed few boundary conditions in U and p files.
But as soon as change the fluid properties to air (rho-1.23, nu 1.47e-5) and solid material properties of polyethylene foam (rho 33, poisson ratio 0.2, E=8.49e+5) keeping freestream conditions the solution crashes after 2 seconds.

Is there anything else I need to consider to look at changing along with these properties that leads to smooth run, since this doesn't seem to a bug?

Enclosed:
log file:
https://drive.google.com/file/d/1wiC...ew?usp=sharing

[bigphil]

Originally Posted by danielparmar

I recently started working on a project related to FSI of flexible wings. I am using turekHron fsi case from solids4foam. Since for flexible wing, atmospheric conditions are needed. Thus I have changed few boundary conditions in U and p files.
But as soon as change the fluid properties to air (rho-1.23, nu 1.47e-5) and solid material properties of polyethylene foam (rho 33, poisson ratio 0.2, E=8.49e+5) keeping freestream conditions the solution crashes after 2 seconds.

Is there anything else I need to consider to look at changing along with these properties that leads to smooth run, since this doesn't seem to a bug?

Enclosed:
log file:
https://drive.google.com/file/d/1wiC...ew?usp=sharing

I suggest starting with a simple version of your case that you can get working and then slowly adding complexity. For example, try using much stiffer mechanical properties to begin with to minimise the effect of coupling and check everything works.

[Neb]

Hi everyone,
I am doing an FSI analysis with solids4Foam of a deformable tube (hyperelastic model). I want the movements on the wall. I used unsNonLinearGeometryTotalLagrangian as solidModel, so I need to understand how it works PointMotionU for both fluid and solid region.

I have already performed a simulation by placing fixedValue for all contours. But I'm not sure I got what I want.

I read in the tutorials documentation that "some of the solidsModel use a non-moving mesh formulation so, by default, some models may not move at all when show in paraview".
What are these solidsModel?

[bigphil]

Originally Posted by Neb

Hi everyone,
I am doing an FSI analysis with solids4Foam of a deformable tube (hyperelastic model). I want the movements on the wall. I used unsNonLinearGeometryTotalLagrangian as solidModel, so I need to understand how it works PointMotionU for both fluid and solid region.

I have already performed a simulation by placing fixedValue for all contours. But I'm not sure I got what I want.

I read in the tutorials documentation that "some of the solidsModel use a non-moving mesh formulation so, by default, some models may not move at all when show in paraview".
What are these solidsModel?

The only solidModels which move the mesh are those that use an updated Lagrangian formulation, so they will have the words UpdatedLagrangian in their name. Note that the total Lagrangian methods are mathematically equivalent but they are formulated so that they can calculate the same deformation field without the need to update the mesh (but of course you can move the mesh in post processing to see the true deformation, if you like). For FSI, it doesn't quite matter which one you use as the deformation field is transferred to the fluid rather than the solid mesh motion.

As regards pointMotionU, it doesn't exist for the solid, and for the fluid you just need to set the interface type to fixedValue and this value gets updated by the FSI procedure (ideally this should be a boundary condition but this is the way it is done for now). The rest of the boundary conditions for the fluid can be set whatever way you like, just like using dynamic mesh in a fluid only case.

[Neb]

Originally Posted by bigphil

The only solidModels which move the mesh are those that use an updated Lagrangian formulation, so they will have the words UpdatedLagrangian in their name. Note that the total Lagrangian methods are mathematically equivalent but they are formulated so that they can calculate the same deformation field without the need to update the mesh (but of course you can move the mesh in post processing to see the true deformation, if you like). For FSI, it doesn't quite matter which one you use as the deformation field is transferred to the fluid rather than the solid mesh motion.

As regards pointMotionU, it doesn't exist for the solid, and for the fluid you just need to set the interface type to fixedValue and this value gets updated by the FSI procedure (ideally this should be a boundary condition but this is the way it is done for now). The rest of the boundary conditions for the fluid can be set whatever way you like, just like using dynamic mesh in a fluid only case.

Thanks for the clarifications. So for the solid region in dynamicFvMeshDict I can only use staticFvMesh?

[MFWilliams]

Hello everyone,

I am in the process of trying to build an FSI simulation to simulate blood flow in an intracranial aneurysm I have a working CFD simulation and am now trying to get a working CSD simulation before I progress onto the full FSI to test my mesh for the solid domain.


However, I cannot get a working CSD simulation to work on my mesh. I started from the pressureisedCylinder fe40 tutorial and have only changed the mesh from the one from the tutorial to the one I am using (attached to this post) and changed the boundary conditions to match the patches for my mesh. I havent changed anything in the fvSolution, fcScheme or controlDict and have only.


But the simulation isnt converging. The output is shown below:

Selecting physicsModel solid

Selecting solidModel linearGeometryTotalDisplacement
Selecting dynamicFvMesh staticFvMesh
Creating fixedDisplacement boundary condition
Creating solidTraction boundary condition
    pressure is time-varying
    limiter coefficient: 1
Creating solidTraction boundary condition
    limiter coefficient: 1
    under-relaxation method: fixed
Creating the mechanicalModel
Selecting mechanical law linearElastic
Creating pointHistory function object.
History point ID: 10664
History point coordinates: (-0.0422648 -0.056142 -0.539776)
Reference point coordinates: (7 0 0)
Time = 10

Evolving solid solver
Solving the momentum equation for D
setCellDisplacements: reading cellDisplacements
    Corr, res, relRes, matRes, iters
    100, 0.96642, 1.85082, 0, 5
    200, 0.99709, 1.82295, 0, 5
    300, 0.997185, 1.8237, 0, 5
    400, 0.997039, 1.82484, 0, 5
    500, 0.996978, 1.82504, 0, 5
    600, 0.997064, 1.82414, 0, 5
    700, 0.997169, 1.82328, 0, 5
    800, 0.997197, 1.82361, 0, 5
    900, 0.997057, 1.82473, 0, 5
    1000, 0.996976, 1.82508, 0, 5
    1100, 0.997054, 1.82428, 0, 5
    1200, 0.997158, 1.82331, 0, 5
    1300, 0.997205, 1.82352, 0, 5
    1400, 0.997075, 1.82461, 0, 5
    1500, 0.996976, 1.82511, 0, 5
    1600, 0.997047, 1.82442, 0, 5
    1700, 0.997146, 1.82336, 0, 5
    1800, 0.997211, 1.82344, 0, 5
    1900, 0.997093, 1.82449, 0, 5
Floating point exception

Does anybody have any ideas how I can get this to run?

[ilhado]

Originally Posted by MFWilliams

Hello everyone,

I am in the process of trying to build an FSI simulation to simulate blood flow in an intracranial aneurysm I have a working CFD simulation and am now trying to get a working CSD simulation before I progress onto the full FSI to test my mesh for the solid domain.


However, I cannot get a working CSD simulation to work on my mesh. I started from the pressureisedCylinder fe40 tutorial and have only changed the mesh from the one from the tutorial to the one I am using (attached to this post) and changed the boundary conditions to match the patches for my mesh. I havent changed anything in the fvSolution, fcScheme or controlDict and have only.


But the simulation isnt converging. The output is shown below:

Selecting physicsModel solid

Selecting solidModel linearGeometryTotalDisplacement
Selecting dynamicFvMesh staticFvMesh
Creating fixedDisplacement boundary condition
Creating solidTraction boundary condition
    pressure is time-varying
    limiter coefficient: 1
Creating solidTraction boundary condition
    limiter coefficient: 1
    under-relaxation method: fixed
Creating the mechanicalModel
Selecting mechanical law linearElastic
Creating pointHistory function object.
History point ID: 10664
History point coordinates: (-0.0422648 -0.056142 -0.539776)
Reference point coordinates: (7 0 0)
Time = 10

Evolving solid solver
Solving the momentum equation for D
setCellDisplacements: reading cellDisplacements
    Corr, res, relRes, matRes, iters
    100, 0.96642, 1.85082, 0, 5
    200, 0.99709, 1.82295, 0, 5
    300, 0.997185, 1.8237, 0, 5
    400, 0.997039, 1.82484, 0, 5
    500, 0.996978, 1.82504, 0, 5
    600, 0.997064, 1.82414, 0, 5
    700, 0.997169, 1.82328, 0, 5
    800, 0.997197, 1.82361, 0, 5
    900, 0.997057, 1.82473, 0, 5
    1000, 0.996976, 1.82508, 0, 5
    1100, 0.997054, 1.82428, 0, 5
    1200, 0.997158, 1.82331, 0, 5
    1300, 0.997205, 1.82352, 0, 5
    1400, 0.997075, 1.82461, 0, 5
    1500, 0.996976, 1.82511, 0, 5
    1600, 0.997047, 1.82442, 0, 5
    1700, 0.997146, 1.82336, 0, 5
    1800, 0.997211, 1.82344, 0, 5
    1900, 0.997093, 1.82449, 0, 5
Floating point exception

Does anybody have any ideas how I can get this to run?

What is the quality of your mesh and what relaxation are you using? Based on the details you gave, I would suspect of a mesh-related issue. Especially in those high-curvature regions you may get some bad cells due to the extrusion (I am supposing you extruded a surface to get the wall mesh) so you would need to use a much smaller relaxation factor to make it converge.

Iago

[MFWilliams]

The output of checkMesh is below and it doesnt seem too bad i thought:

Overall number of cells of each type:
    hexahedra:     7004
    prisms:        20
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     28

Checking topology...
    Boundary definition OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
    Patch               Faces    Points   Area [m^2]  Surface topology
    solidEnds           148      222      8.2858e-06  ok (non-closed singly connected)
    fluidInterface      3526     3566     0.000360889 ok (non-closed singly connected)
    outerSolidFace      3526     3566     0.000429082 ok (non-closed singly connected)

Checking geometry...
    This is a 3-D mesh
    Overall domain bounding box (-0.0526934 -0.0692914 -0.550554) (-0.0422648 -0.0550044 -0.532973)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Mesh (non-empty, non-wedge) dimensions 3
    Boundary openness (-8.6567e-18 2.50292e-17 -3.33004e-17) Threshold = 1e-06 OK.
    Max cell openness = 2.31715e-16 OK.
    Max aspect ratio = 4.43331 OK.
    Minumum face area = 7.2672e-09. Maximum face area = 4.09604e-07.  Face area magnitudes OK.
    Min volume = 1.27823e-12. Max volume = 5.71463e-11.  Total volume = 1.25617e-07.  Cell volumes OK.
    Mesh non-orthogonality Max: 59.9269 average: 11.5378 Threshold = 70
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 1.09335 OK.

I extruded the outer surface which was one single patch to get the wall mesh. The relaxation factor in fvSolution which I am using is 0.9 for fields "D|DD" and I'm not using one for the equations.

[MFWilliams]

Also what is the purpose of the point history function that is written as reference point coordinates in the initial output from running the solver?

[ilhado]

Originally Posted by MFWilliams

The output of checkMesh is below and it doesnt seem too bad i thought:

Overall number of cells of each type:
    hexahedra:     7004
    prisms:        20
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     28

Checking topology...
    Boundary definition OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
    Patch               Faces    Points   Area [m^2]  Surface topology
    solidEnds           148      222      8.2858e-06  ok (non-closed singly connected)
    fluidInterface      3526     3566     0.000360889 ok (non-closed singly connected)
    outerSolidFace      3526     3566     0.000429082 ok (non-closed singly connected)

Checking geometry...
    This is a 3-D mesh
    Overall domain bounding box (-0.0526934 -0.0692914 -0.550554) (-0.0422648 -0.0550044 -0.532973)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Mesh (non-empty, non-wedge) dimensions 3
    Boundary openness (-8.6567e-18 2.50292e-17 -3.33004e-17) Threshold = 1e-06 OK.
    Max cell openness = 2.31715e-16 OK.
    Max aspect ratio = 4.43331 OK.
    Minumum face area = 7.2672e-09. Maximum face area = 4.09604e-07.  Face area magnitudes OK.
    Min volume = 1.27823e-12. Max volume = 5.71463e-11.  Total volume = 1.25617e-07.  Cell volumes OK.
    Mesh non-orthogonality Max: 59.9269 average: 11.5378 Threshold = 70
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 1.09335 OK.

I extruded the outer surface which was one single patch to get the wall mesh. The relaxation factor in fvSolution which I am using is 0.9 for fields "D|DD" and I'm not using one for the equations.

Yep, the mesh is fine, but from my experience with these geometries, you should use a smaller field relaxation factor. For example, I found an optimum value of 0.5-0.7 for the cases I ran (using nonlinear laws and realistic material properties for aneurysms).

Apart from that, there are several other factor that may affect your solution. To try to get a first converging case, I would also recommend you use a larger elastic modulus (so you get smaller deformations) and change the inner pressure BC (it may be too high depending on the tutorial you extracted the case from). Try to directly use some realistic values for this pressure considering the human cardiac cyle, like an average of 100 mmHg.

Also, check the Poisson ratio you are using. If trying to achieve the incompressible behavior (with nu -> 0.5) then the solution may take a lot of iterations to converge, if it converges at all. Try something smaller at first, eg nu between 0.45 and 0.48, it may give some more reasonable computational times. And activate the solution of the pressure diffusion equation in s4f, that helps to quells any oscillations in the solution.

Finally, and related to the pressure oscillations problem that may cause the divergence you are getting, I suggest you to use triangular prismatic cells in the wall, instead of hexahedral ones. Apparently, pressure oscillations are more prone to occur in quadrilateral meshes than in triangular ones (for the 2D case) when using displacement-based solvers with the Finite Volume Method (check this paper
"Wheel MA. A mixed finite volume formulation for determining the small strain deformation of incompressible materials. International Journal for Numerical Methods in Engineering. 1999;44:1843–61"). Briefly, I was using hexahedral meshes, like yours, and once changed to triangular ones, several cases that were stubbornly diverging, due to the pressure oscillations in small regions, finally worked.

Hope this helps!
Iago

[MFWilliams]

Originally Posted by ilhado

Yep, the mesh is fine, but from my experience with these geometries, you should use a smaller field relaxation factor. For example, I found an optimum value of 0.5-0.7 for the cases I ran (using nonlinear laws and realistic material properties for aneurysms).

Apart from that, there are several other factor that may affect your solution. To try to get a first converging case, I would also recommend you use a larger elastic modulus (so you get smaller deformations) and change the inner pressure BC (it may be too high depending on the tutorial you extracted the case from). Try to directly use some realistic values for this pressure considering the human cardiac cyle, like an average of 100 mmHg.

Also, check the Poisson ratio you are using. If trying to achieve the incompressible behavior (with nu -> 0.5) then the solution may take a lot of iterations to converge, if it converges at all. Try something smaller at first, eg nu between 0.45 and 0.48, it may give some more reasonable computational times. And activate the solution of the pressure diffusion equation in s4f, that helps to quells any oscillations in the solution.

Finally, and related to the pressure oscillations problem that may cause the divergence you are getting, I suggest you to use triangular prismatic cells in the wall, instead of hexahedral ones. Apparently, pressure oscillations are more prone to occur in quadrilateral meshes than in triangular ones (for the 2D case) when using displacement-based solvers with the Finite Volume Method (check this paper
"Wheel MA. A mixed finite volume formulation for determining the small strain deformation of incompressible materials. International Journal for Numerical Methods in Engineering. 1999;44:1843–61"). Briefly, I was using hexahedral meshes, like yours, and once changed to triangular ones, several cases that were stubbornly diverging, due to the pressure oscillations in small regions, finally worked.

Hope this helps!
Iago

Thank you for your reply.


I was unaware of the effect that poissons ratio could have but I was already using a value of 0.45 for relaxation factor but I have now tried a simulation with a relaxation factor of 0.6 for D|DD, an elastic modulus of 1.6e+12 and realistic pressure ranging from 0 to 16000Pa in 5 seconds. It converged much better with the relaxation factor of 0.6, now only taking around 2200 corrector steps. I had assumed 0.1 would give the best convergence but obviously not as that was taking around 18000 corrector steps and barely converging.

Time = 5

Evolving solid solver
Solving the momentum equation for D
    Corr, res, relRes, matRes, iters
    100, 0.000824979, 0.00622766, 0, 8
    200, 0.000558005, 0.00313425, 0, 7
    300, 0.00041514, 0.00202222, 0, 10
    400, 0.000324802, 0.00140024, 0, 16
    500, 0.000263683, 0.00101591, 0, 16
    600, 0.000219222, 0.000774099, 0, 16
    700, 0.000186184, 0.000595204, 0, 16
    800, 0.000160003, 0.00047062, 0, 17
    900, 0.000137416, 0.000387662, 0, 17
    1000, 0.00012029, 0.000345773, 0, 18
    1100, 0.000107792, 0.000299383, 0, 18
    1200, 9.00661e-05, 0.000248215, 0, 16
    1300, 7.49945e-05, 0.000209708, 0, 15
    1400, 5.95477e-05, 0.000163253, 0, 6
    1500, 4.39609e-05, 0.000201844, 0, 1
    1600, 4.15789e-05, 6.73362e-05, 0, 5
    1700, 3.46355e-05, 0.000170922, 0, 1
    1800, 2.54326e-05, 0.000118597, 0, 5
    1900, 2.14851e-05, 0.000183497, 0, 1
    2000, 1.84945e-05, 6.22462e-06, 0, 1
    2100, 2.28104e-05, 6.42462e-06, 0, 1
    2200, 1.02707e-05, 6.42421e-05, 0, 3
    The relative residual has converged
    2216, 9.8153e-06, 0, 0, 0

Max epsilonEq = 3.88914e-07
Max sigmaEq (von Mises stress) = 643720
ExecutionTime = 212.19 s  ClockTime = 214 s

Also just to confirm, for a solid case such as this, when I am specifying a time varying pressure, should I specify the pressure divided by the density or the absolute pressure?


That is very interesting about the tet mesh and its effects and I will give that a go but it will take slightly longer.



Thank you very much for your help and I will hopefully reply soon with the result of the tetrahedral mesh

[MFWilliams]

Do you know of a method that would be able to create a tetrahedral mesh for the solid domain and make sure that it is coherant with the fluid domain given that the fluid domain was created on cfMesh?


Merlin

[treem22]

Originally Posted by MFWilliams

Thank you for your reply.
Also just to confirm, for a solid case such as this, when I am specifying a time varying pressure, should I specify the pressure divided by the density or the absolute pressure?

My understanding is that it is the absolute pressure. Working with kinematic pressure (https://www.openfoam.com/documentati...-pressure.html) is only relevant when using incompressible fluid solvers in OpenFOAM.

Originally Posted by MFWilliams

Do you know of a method that would be able to create a tetrahedral mesh for the solid domain and make sure that it is coherant with the fluid domain given that the fluid domain was created on cfMesh?

What do you mean by "coherant"? If you mean that the meshes must share nodes at the fluid-solid interface, then I don't know of any method that you can use outside of a commercial meshing program. I struggled with this as well, and didn't have the extra requirement of my meshes be entirely tets. I ended up using multi-region meshing workflows for snappyHexMesh, but that doesn't really help you because it will create hexes instead of tets. I know it can be done in Pointwise, but that's a commercial code.

[MFWilliams]

Originally Posted by treem22

My understanding is that it is the absolute pressure. Working with kinematic pressure (https://www.openfoam.com/documentati...-pressure.html) is only relevant when using incompressible fluid solvers in OpenFOAM.



What do you mean by "coherant"? If you mean that the meshes must share nodes at the fluid-solid interface, then I don't know of any method that you can use outside of a commercial meshing program. I struggled with this as well, and didn't have the extra requirement of my meshes be entirely tets. I ended up using multi-region meshing workflows for snappyHexMesh, but that doesn't really help you because it will create hexes instead of tets. I know it can be done in Pointwise, but that's a commercial code.

Ok thank you for confirming that about specifying the pressure. Although which pressure does solids4Foam use, kinematic or absolute?


And yes sorry I did mean that they must share nodes. Ok I'm not completely against commercial meshers as through my university I have access to pointwise, and I can get access to the Ansys student software. So you think adding a tetrahedral solid domain to an already created hexahedral mesh of the fluid domain is possible in pointwise?


Thank you,
Merlin

[bigphil]

Originally Posted by MFWilliams

Although which pressure does solids4Foam use, kinematic or absolute?

Are you referring to the solid or the fluid?
Like in OpenFOAM, some fluid solvers (fluid models) uses kinematic pressure (incompressible ones) and some use pressure in Pascals.
For the solid models in solids4foam they all use pressure in Pascals.
The FSI coupling procedure will convert the fluid kinematic pressure to pressure when transferring to the solid, if needed.

Originally Posted by MFWilliams

And yes sorry I did mean that they must share nodes. Ok I'm not completely against commercial meshers as through my university I have access to pointwise, and I can get access to the Ansys student software. So you think adding a tetrahedral solid domain to an already created hexahedral mesh of the fluid domain is possible in pointwise?

One option is to create your fluid mesh (e.g. using cfMesh or snappyHexMesh) and then use the OpenFOAM utility extrudeMesh to "extrude" the solid mesh from the fluid interface patch.

[MFWilliams]

Originally Posted by bigphil

Are you referring to the solid or the fluid?
Like in OpenFOAM, some fluid solvers (fluid models) uses kinematic pressure (incompressible ones) and some use pressure in Pascals.
For the solid models in solids4foam they all use pressure in Pascals.
The FSI coupling procedure will convert the fluid kinematic pressure to pressure when transferring to the solid, if needed.



One option is to create your fluid mesh (e.g. using cfMesh or snappyHexMesh) and then use the OpenFOAM utility extrudeMesh to "extrude" the solid mesh from the fluid interface patch.

Sorry, I meant for the fluid domain which pressure does solids4Foam use. So for example, adapting the 3dTube case, which pressure should be used in the BC?


That meshing workflow is what I am currently using but is it possible to specify the element types using extrudeMesh? As I wanted to try create the solid domain using tetrahedral elements because of what Iago said that it can help pressure oscillations.

[bigphil]

Originally Posted by MFWilliams

Sorry, I meant for the fluid domain which pressure does solids4Foam use. So for example, adapting the 3dTube case, which pressure should be used in the BC?

Like for standard OpenFOAM fluid solvers, the type of pressure used depends on the chosen fluid solver (or fluid model in solids4foam).
In the solids4foam/tutorials/fluidSolidInteraction/3dTube/3dTube case, icoFluid (i.e. icoFoam approach) is used, so "p" is kinematic pressure. You can check this for any case by examining the dimensions of the p field in the 0 directory.

Originally Posted by MFWilliams

That meshing workflow is what I am currently using but is it possible to specify the element types using extrudeMesh? As I wanted to try create the solid domain using tetrahedral elements because of what Iago said that it can help pressure oscillations.

I believe Iago was suggesting to use triangular prisms for the solid, i.e. if the fluid interface has triangles then the extruded mesh will be triangular prisms. extrudeMesh just extrudes the patch 2-D cells so it does not have any control over the type of cells created; it just creates extruded layers of a surface mesh.